Random Vibration (PSD) Analysis Using Ansys Mechanical

Hi everyone, today I'm going to be giving you a quick run through on how to do a PSD analysis using ANSYS Mechanical. So first in ANSYS Workbench, we need to set up a modal analysis and a random vibration analysis.

To do this, drag and drop from the solution block in modal to the setup block in random vibration. This will import the results of the modal into the setup for the random vibration analysis.

In the right image, we can see that under the random vibration branch in the tree in the mechanical interface, the modal results are shown there as the initial condition for the random vibration.

As far as loads and supports go, in the modal analysis, we need to define some kind of support on our model. This can either be a fixed support, a displacement, or a remote displacement.

For the random vibration analysis, we're going to be setting up some sort of PSD base excitation and this is going to be scoped to the support that we defined in the modal analysis. For the PSD curve and the random vibration, it's a piecewise linear frequency table.

As the user, we define a series of plots or a series of points of PSD over frequency. There are a couple of ways we can do this. For example, for the random vibration analysis, we're going to need the maximum frequency.

To find this, we can take a point, find the maximum frequency of that point, and then use linear interpolation to fill in the rest of the curve.

Under analysis settings, in modal analysis, we want to take whatever the highest frequency in our PSD curve is, and multiply that by 1.5 and make that our maximum frequency in the range.

We want to go from 0, we want the frequency range to go from 0 to 1.5 times the maximum frequency in our PSD curve. In random vibration, we want to set the number of modes to use, set that to all. Under exclude insignificant modes, set that to yes. Then, define a mode significance level.

This will exclude some of the modes from the modal solution that are below whatever the significance level is, which is also known as the participation factor. Any modes found in the modal analysis that are below this participation factor will not be solved for in the random vibration.

That's it for the setup. After solving, we can look at the results. Since this is a statistical solution, not all results will be available. However, we can still look at the displacement, velocity, and acceleration.

We can also look at the vibration directional components, normal and shear stress and strains, and the equivalent stress. Here is a sample project that I've set up. I've linked the engineering data, geometry, and model of a modal to a random vibration, as well as the solution to the setup.

In the analysis settings of modal, I've set max modes to find 250. I've linked the data geometry and model to a random vibration. I've set the range from 0 to 4500 Hertz. The reason being that my PSD curve goes up to 3000 Hertz. I have a fixed support just on this back face here.

After solving the modal analysis, we can look under random vibration analysis settings. The number of modes to use is all, exclude insignificant modes is yes, and I've set the mode significance level to 1e- 4. The PSD curve I've chosen looks like this. After solving, I have a couple of plots here.

This is the directional deformation, and we can also look at stresses and strains, as well as define a response PSD. Thank you very much for your attention. Here at Ozen Engineering, we use physics-based simulation to solve multidisciplinary engineering problems.

We specialize in FEA, CFD, and high and low frequency electromagnetics.

If you're interested in learning more about ANSYS software or talking to us about our consulting services, you can email us at [info@ozeninc.com](mailto:info@ozeninc.com), call our office phone number, or visit our website at [ozeninc.com](http://ozeninc.com).

Reference(s): title: Random Vibration (PSD) Analysis Using Ansys Mechanical